## General Mechanical

#### Problem in membrane stress

• oumaimalahmar.ol
Subscriber

Hello,

@peteroznewman

Can you help me I'm working on a tank, I did the mesh convergence to get my results, for example with a bottom thickness of 5mm and a mesh convergence I find that my membrane stress is equal to 209MPa and as soon as I increase the thickness to 6mm with the convergence I find a stress of 250MPa which is not logical at all the stress should normally decrease I don't know what the problem is.

• peteroznewman
Subscriber
There is not enough information in your post to understand the tank geometry and supports.
You show a Displacement convergence graph. Displacement converges faster than stress. How do you know the stress converged?
• oumaimalahmar.ol
Subscriber
there is my complete model,
I applied a fixed support at the top and bottom of the tank, a pressure inside the tank of 0.005MPa and a force of 4.73e+5 MPa on the bottom of the tank.
it is not better to do my convergence study on the constraints which are elementary results contrary to the displacements which are "exact" nodal results, that is why I did the convergence on the displacement and I look at the constraints.
I work on the same model when I increase the thickness of the bottom the stress also increases when I do the convergence and without convergence the stress decreases something I did not understand

• peteroznewman
Subscriber
The Fixed Supports are introducing an artificial stress concentration into the model that is not present in the real world.
In reality, what supports the top and bottom of the tank?
There are methods of creating constraints to allow Static Structural to solve without introducing artificial stress concentrations.
For example, a Remote Displacement, Behavior = Flexible, could be used on the bottom circle. All six DOF should be set to zero.
Why do you need a Fixed Support on the top of the tank? Try solving with that suppressed.
Displacement will converge in a model that includes a Stress Singularity. Stress will not converge in such a model. If you are interested in stress, you must do the mesh refinement study on stress.
You could create a 2D Axisymmetric model and have elements through the thickness of the walls to see detailed stress concentrations if the geometry is axisymmetric.
• oumaimalahmar.ol
Subscriber
Hello, i understand you, i use a fixed support on the top of the tank to take into account the effect of the cover.
it is better not to do my convergence study on the constraints which are elementary results contrary to the displacements which are "exact" nodal results that's why. you find the complete geometry of my model.
Thank you

• peteroznewman
Subscriber
Your model should include the cylindrical support barrel below the bottom of the tank. The fixed support can be on the bottom of that cylinder and you can ignore the stress around the fixed support.
Your model should include the cover. The cover is flexible while a fixed support is not, so the fixed support does not give a good result for the stress at the top of the tank.
• oumaimalahmar.ol
Subscriber

I did not understand what you mean bythe cylindrical support barrel, instead of applying the fixed support on the edge of the skirti apply a remote displacement and i took the cover, but always the same problem,
• oumaimalahmar.ol
Subscriber
what I noticed that the singularity of the constraints is caused by the contact
when i don't create the contact on workbench and I use the parter option on spaceclaim my model converges but it's correct what i do i dont take into account of the contact knowing that i have a totally linked contactin my model.

• peteroznewman
Subscriber
The last image helped me to understand that your model does include the cylindrical support barrel.
If the bottom of the tank is welded to the support barrel, then using Shared Topology in SpaceClaim and having no contact is an accurate model.
If the bottom of the tank is sitting on the support barrel, then frictional contact is appropriate. If you are getting stress concentrations, you might need more detailed geometry to more accurately represent the stress.
You could create a 2D Axisymmetric model and have elements through the thickness of the walls to see detailed stress concentrations if the geometry is axisymmetric.
• oumaimalahmar.ol
Subscriber
normally the bottom is welded to the support barrel,
my manager wants me to work with the complete model dont use the axisymmetric.
thank you for your response i want just know the way ANSYS treats parts with shared topology is like a bounded contact.
• peteroznewman
Subscriber
Shared topology is the best option to cleanly connect two parts that have a continuous, full-penetration weld joining them.
Bonded contact is less desirable because there may be more or less nodes connected depending on the pinball radius and the varying location of nodes on each part.
• oumaimalahmar.ol
Subscriber
Thank you so much